Top-down asembly design. What are you guys using now?

[Patriot_1776]

Well, being an Olde Timer here, I remember when "Layout/Notebook" (If I remember the proper terms) was the hot ticket method promoted by PTC.  Then they went to the "Master Model" method.  Then there's the "Skeleton" method.  I used the "Master" model technique a couple times in the early 2000's, but had some issues with it, especially with layers.  Then I switched to using Skeleton models, and while I had some issues with layers in the early 2010's, it seems to work now.  I DON'T like the fact that (at least from what I remember - that may have changed) the Skeleton doesn't always travel with the related submodels like the Master model always did.  So, I use the Skeleton method now because of the issues I had using the Master model method.

What are you guys using and why?  We're writing a spec for our group regarding modeling practices and dwgs, and we want to include top-Down design.

Grazie!

[tbraxton]

It seems PTC has all but abandoned notebook (*.lay files). I would love to see them further developed. I have only used a notebook once in the last 3 years but it let me solve a problem requiring anisotropic scaling of geometry completely within Creo Parametric vs using an external application to do the math needed to develop and manage relations to modify a design model into a tooling release model (they are not geometrically congruent). Mathcad could also do this BTW but if you have the math functions required in Creo I would pick a notebook over Mathcad to manage things.

We use all of the top-down design tools available including layouts (now Notebook files). I would add that in Creo 7+ multibody is available and can be used in a top-down paradigm. The multibody can replace surface master models in some cases and is advantageous in this context because it can be done faster than pure surface modeling with multibody sometimes. I do not consider it a replacement for the master model merge technique but rather an enhancement.

For multi-domain geometry creation (i.e., gas volume in contact with liquid volume) it is so fast to create geometry driven by a single master model and then split them out to individual derivative parts. PTC demos show multi-material (i.e., 2 shot molding) but it has a lot of utility to create geometry used for CAE quickly.

Our first real use of multibody was for some injection molded fluid handling components that were designed from the inside out (optimized wetted surfaces and flow volumes). The interior volumes were optimized with CFD and FEA and then the fluid master bodies were developed into injection molded parts with constant wall thickness shells. Multibody allowed us to complete this work and support the simulation with less hours of work to create and modify the 3D models throughout development vs without.

[Patriot_1776]

'Sup Tom!

Huh, while you have an excellent post, I didn't mark it as the "Solution".  PTC must have done it.  Perhaps they bought one of Hunter's paintings???🤣

I DO miss doing IM plastic work, that was the most challenging stuff I've ever done, it was fun!  I did a couple overmold designs over the years, and thought it was really cool!  Sounds like you guys use way more tech stuff than we did.  I think we only did moldflow analysis on one, maybe 2 or 3 of the parts I ever did.

I think for the more simplified stuff we're doing (mostly machined parts), that skeleton works fine, but I liked the Master Model technique if they would have worked the kinks out of it.  I'd like to see them really pick one method and REALLY make it work well....but then, I'm STILL waiting for them to fix the serious "Creo splits everything in half" bug...

Great post, thanks!

[HamsterNL]

We are use INPUT parameters and EXECUTE statements to drive our assemblies. We use Excel to calculate all sorts of parameters (width, height, nr of holes, starting positions, which fasteners to use, etc). We drive our main assembly with 1500+ parameters, but we can update our models with two mouseclicks (one in Excel to write all the parameters to a textfile, one in Creo to read those parameters from that textfile).

We use Family Tables, Interchange Assemblies, Component Interfaces and Copy/Publish Geometry.

We can reuse (almost) any part because they are all driven by INPUT parameters (and we can redefine the source of a Copy Geometry to a different one).

I wish that Notebooks would give me the option to import/declare only a sub-set of all the parameters into a part, but that's not possible at this time.

https://community.ptc.com/t5/3D-Part-Assembly-Design/Creo-Notebooks-Import-Declare-only-a-few-parameters/m-p/588879

https://community.ptc.com/t5/Creo-Parametric-Ideas/Creo-Notebook-Declare-only-a-few-parameters-not-all-parameters/idi-p/590645